GSK GSK988TA, Manual

Page: 116 / 531

GSK988TA/GSK988TA1/GSK988TB Turning Center CNC System User Manual 【 Programming & Operation 】
98
Ⅰ
Programming
(X40), Z tool infeed 3mm and cycle the above-mentioned
steps to continuously run programs
）
G0 X150 Z50
； （
Return to start point of machining
）
M30 ； （ End of program ）
2.19.7 Notes for Multi Cycle Machining
Note 1. When the multi cycle blocks are executed, they should be the specified address P, Q, X, Z, U, W, R of
each block;
Note 2. The block specified by P in G71
，
G72, G73 should be G00 or G01. When there is no code, the system
alarms;
Note 3. In MDI and DNC mode, G70
，
G71
，
G72 or G73 can not be specified, otherwise, an alarm occurs. But in
MDI and DNC mode, G74
，
G75 or G76 can be specified;
Note 4: The block quantity of G70, G71, G72 or G73 in the sequence numbers specified by P and Q cannot
exceed 100;
Note 5: The blocks in the serial numbers specified by P and Q in G71
，
G72 or G73 cannot specify the following
code:
（
1
）
non-modal G code except for G04 in group 00;
（
2
）
all G codes except for G00, G01, G02, G03 in group 01;
（
3
）
G20 and G21;
（
4
）
M98 and M99;
Note 6: The skip function should not be executed in the blocks of their serial number specified by P and Q.
when the skip function is used in the blocks of their serial numbers specified by P and Q.
Note 7: The tool nose radius compensation is invalid in G71 ～ G76.
Note 8: No.5104 Bit2 (FCK ） sets whether G71, G72 or G73 executes the outer check. When it is set to1, the
check is executed. The system alarms when the positioning point is in the cutting range.
Note 9: No.5102 Bit1 （ MRC ） set whether the system alarm when the finishing cycle in G71 ， G72 is in
non-monotonous, and an alarm occurs when Bit1 is set to 1.
2.20 Threading Cutting
GSK988TA/AB CNC system can machine many kinds of thread cutting, including metric/inch
single, multi threads, thread with variable lead and tapping cycle. Length and angle of thread run-out
can be changed, multiple cycle thread is machined by single sided to protect tool and improve smooth
finish of its surface. Thread cutting includes: continuous thread cutting G32, thread cutting with
variable lead G34, Z thread cutting G33, Thread cutting cycle G92, Multiple thread cutting cycle G76.
The machine used to thread cutting must be installed with spindle encoder, the transmission ratio
between spindle and encoder is set by the parameter. There are two kind of communication
connection method. The encoder data is transferred to the CNC by the servo spindle in bus
communication mode or the spindle encoder is connected with the CNC by the encoder wires. X or Z
traverses to start machine after the system receives spindle signal per rev in thread cutting, and so
one thread is machined by multiple roughing, finishing without changing spindle speed.
GSK988TA/TB CNC system can machine many kinds of thread cutting, such as thread cutting
without tool retraction groove. There is a big error in the thread pitch because there are the
acceleration and the deceleration at the starting and ending of X and Z thread cutting, and so there is
length of thread lead-in and distance of tool retraction at the actual starting and ending of thread
cutting.
X or Z traverse speed is defined by spindle speed instead of cutting feedrate override in thread